Ally 6061 Deep Box Machining - cutters / strategy

[Newbeeee™]

So we're making a job that is 4" x 4" x 3.5" deep inside.

There's plenty of detail inside and we're roughing it out with a 1/2" MAFord knuckle style long series.

All okay.

We're also chain drilling all inside corners where we can as there is a 1/4" slot sat against a sidewall, right at the bottom.

The inside can be finished with a 5/16" cutter.

The 1/4" slot can be finished with a 1/4" cutter (full slot ramp back and forth) or a 6mm (slightly smaller) and spiral ramp.

For cutters, I'm thinking solid carbide (obviously) higher helix as possible with short length flute, and no neck reduction (strongest possible shank). Also as sharp bottom geometry as possible - no edge sweeper/flat, so the cutting is as keen as poss.

5/16" cutter DOC's are only going to be about .040" waterlining  after the 1/2" rougher, at say S6000 F40"/min.

For any full width slotting - DOC 10thou and high speed it?

 

Does it all sound okay?

Any wisdom from anyone (please!).

Any fave cutters for this type of work?

 

The roughing is all done - we're struggling with the 5/16" to get a finish. Haven't got to the 1/4" yet...

 

[rdsnx]

What are your benching options after part is machined. In other words, would a mismatch resulting from using two different cutters to finish be acceptable. If so, I'd finish with a larger cutter and ramp mill corners and REST with 5/16 mill.

[Newbeeee™]

Ray,

Polishing is okay to do (but we don't want to if we can avoid it).

Biggest problem is only a 24tool changer and there's a ton of different threads in the part as well!

cheers

[rdsnx]

For feeds and speeds consider Harvey's catalog. They specialize in extra long cutters. I'm not accustomed to using their website, but I know their catalog has pretty good numbers for extra longs.

http://www.harveytool.com/cms/SpeedsFeeds_228.aspx

 

good luck

[crazy^millman]

I am a big Helical fan and have been using their long reach tools with very good success. I have been using 5 flute endmills for finishing walls with no problem. Right now I am taking a 3/4 5 flute endmill on 7075-T851 with .025 of stock. DOC is 2.5 at 4000 rpms and 40 imp. Finish is 32 all day long.

 

My friend over at Reid talked me into trying it and people always want to go to 2 flute or 3 flute for fishing aluminum, but forget about the core strength loss on the less flutes. The more flutes the stronger the core of the tool is. The stronger the core of the tool is the less deflection and the less problems with chatter from the tool.

 

Just my thoughts on this topic. Got a Model then I can give other ideas.

[Newbeeee™]

Thanks Ron - its 10meg.

If I email it to 5thaxis, it's 10meg. Is this okay?

Cheers

[crazy^millman]

Yes sir. Be glad to take a look at it for you.

[rhino44]

Ron. I do a fair amount of deep pocket milling like you have described here. We are currently using Data Flute end mills but I am not here to sell you a tool. My recommendation is to slow your spindle speed to roughly half of what you would normally use for this material, and then I would reduce your depth of cut to the least amount that you can take without pissing off every one above you. You will have to find that happy medium between a 84 hour cycle time and crappy finish. PLay around with back plot until you have a depth of cut and a cycle time that you can live with. Long tools don't like high spindle speeds. Let me know how it turns out.

[Machineguy]

For finishing deep pockets and thin walls we usually relieve the flutes on a long end mill. That stops the rubbing and most of the vibration. The second thing we did was pot the part so the walls are supported on the opposite side. It's a little work to set up but you can run at full speed.

 

Machineguy

[crazy^millman]

Ron. I do a fair amount of deep pocket milling like you have described here. We are currently using Data Flute end mills but I am not here to sell you a tool. My recommendation is to slow your spindle speed to roughly half of what you would normally use for this material, and then I would reduce your depth of cut to the least amount that you can take without pissing off every one above you. You will have to find that happy medium between a 84 hour cycle time and crappy finish. PLay around with back plot until you have a depth of cut and a cycle time that you can live with. Long tools don't like high spindle speeds. Let me know how it turns out.

 

Not sure where in the world you got that 84 hour cycle time and was talking more about the type of tool being 5 flute than 3 flute for finishing. The few seconds it is taking for the tool to walk around the part with a full depth of cut works for me and our customers. They get to tolerance nice looking parts. I normally run max RPM's and on this application that would be 8000 rpms. I cut that by half to 4000 rpms which also means I would have finished it at 80 imp, but again cut that by half so I was already doing what you suggested problem was you were not sitting next to me as I was proving out this project. Part looks amzaing and customer is happy so that is how it turned out. :scooter:

[Newbeeee™]

So we're making a job that is 4" x 4" x 3.5" deep inside.

There's plenty of detail inside and we're roughing it out with a 1/2" MAFord knuckle style long series.

All okay.

We're also chain drilling all inside corners where we can as there is a 1/4" slot sat against a sidewall, right at the bottom.

The inside can be finished with a 5/16" cutter.

The 1/4" slot can be finished with a 1/4" cutter (full slot ramp back and forth) or a 6mm (slightly smaller) and spiral ramp.

For cutters, I'm thinking solid carbide (obviously) higher helix as possible with short length flute, and no neck reduction (strongest possible shank). Also as sharp bottom geometry as possible - no edge sweeper/flat, so the cutting is as keen as poss.

5/16" cutter DOC's are only going to be about .040" waterlining  after the 1/2" rougher, at say S6000 F40"/min.

For any full width slotting - DOC 10thou and high speed it?

 

Does it all sound okay?

Any wisdom from anyone (please!).

Any fave cutters for this type of work?

 

The roughing is all done - we're struggling with the 5/16" to get a finish. Haven't got to the 1/4" yet...

 

So, a little feedback. Job is running sweet but isn't that fast.

The MA Ford style cutter works really well and has eaten the inside.

We restmilled with a 10mm dia 40degree 2x flute which is not relieved. This runs 1/16th DOC at S7200 F80.

The 5/16 follows where it needs and works okay.

The 1/4 slots are chaindrilled first, and then the 1/4" tool follows on centreline and then waterlines the profile. This again is a 40deg 2 flute (short flute) but solid with no relief. The tool does rub the sidewall but is supported and is a whole lot better than a relieved tool. This tool is protruding 3.55" inches (15x d).

This runs at 3thou DOC S8000 and a feed of 30 inch/min. Yes slow, but it gives a good finish.

We tried half a dozen test pieces of all S+F combinations and DOC combinations and toolholder combinations, and this was the best we came up with.

Regarding toolholders, I thought the Schunk Hydraulic would be the best as it is full dia grip and oil damped (so to speak).

Showa Micron chuck was no better.

Shrink rang like a church bell!

Nope. The best by far was a standard ER25 collet chuck with a standard collet. The damping was far greater and the surface finishes (at the same S+F and DOC) were 2 or 3 times better.